Help with multiple passes

[Graham Waterworth]

Hi Sage,

the circle code starts and finishes at the same point so it has no need to rapid up and down, the line M98 P0005 L51 tells the main program to call the sub program O0005 51 times.

Here is a commented snippet of your code.

N2 M6 T2(TOOL Change 1/4 centercut endmill)
G43 H2
G0
M3
 (1ST SLOT)
X4.7834 Y4.0789 (move to start of slot)
Z.600                 (move clear of part by 600 thou)
M98 P0002 L51    (call sub O0002 51 times)
G00 G90 Z.6       (change to absolute and rapid clear)
 (2ND SLOT)
(code removed)
........
M1
M30

O0002 (FIRST SUB)
G00 G91 Z-.6         (set to incremental and rapid to -600 thou)
G1 Z-.01  F.50       (feed into job)
G90                      (set to absolute)
G2 X4.2265 Y3.6499 I-1.9342 J1.9351 F4.00 (create arc)
G0 G91 Z.6           (set to incremental and rapid up 600 thou)
G90 X4.7834 Y4.0789 (rapid back to start of arc)
M99                     (go back to main program)

Any questions just ask.

Graham.

[ger21]

If your using AutoCAD 2002 or newer, I wrote a macro that exports g-code directly from AutoCAD. Far easier than trying to figure out LazyCAM, imo.

http://home.comcast.net/~cncwoodworker/acad/downloads/AC2GCv039.zip

There's more info on it at CNC Zone.
http://www.cnczone.com/forums/showthread.php?t=8226

[Sage]

Graham:

Just to be sure I understand your code, and in the interest of understand the action of the G codes presented:
Do I detect a problem with your approach if the material is greater than 0.6" thick?

It appears you raise the tool a fixed distance of 0.6 inches from it's current depth at the end of each pass which is getting increasingly deaper with each pass. For this example the material is only 0.5" thick so you will be raising it 0.6" above the work surface at the start and only 0.1" on the last pass. Not a problem in this case but I'd lke to understand the codes fully. Perhaps there is something in the absolute / relative feature that makes this non-issue ?

 Am I missing something?

Thanks


Sage
 

[Sage]

ger21:

I'll check out your macro

Thanks


Sage

[Graham Waterworth]

Hi Sage,

you are correct in what you say, that is the main problem of incremental code, as the code is written to do that job then the code is safe, if it is to be adapted for other jobs then all the rapid moves have to be checked and adjusted for safe movement.

If this was going to be a regular problem then the g-code can be written using # codes to allow the code to be altered by the changing of a variable.

CNC is about repetition, we write a g-code program and prove it works, we then save it for the next time we make the same part, if the code worked the first time it will work time and again. 

As with lots of things in this world there are many ways to do a job, finding a way that suites your way of working is the hard bit.

You have learned a lot from this exercise already, just think what you may learn tomorrow.

Graham.